> So, to keep copper from the board edge on the inner planes, which is not a
> bad idea :-), one places track around the board edge. Conveniently, as
> noted by another, this can be nothing more than a blown up version of the
> keepout or board outline. I've always placed this on the plane layers, and
> have tolerated, reluctantly, the Protel warning of inner plane primitives.
> But the CAM Manager would allow the setup of special plot instructions for
> individual layers, and we could assign one of the new mech layers to inner
> plane edge clearance, and plot it together with all the inner planes, thus
> generating no spurious warning. I've not actually done this, however....
> Abdulrahman Lomax

The idea of putting tracks on a Mechanical layer, and then including the
contents of that (Mechanical) layer with just *some* of the Gerber files
produced, to wit, the (Gerber) files produced from the internal power plane
layers (only), raises the issue of a hobby-horse of mine.

The fact that the Gerber files produced from the *other* layers will not
include the contents of the Mechanical layer concerned implies that two sets
of Gerber files need to be produced; these sets are distinct because the set
of Mechanical layers which are included with each Gerber file depends upon
which layer that the Gerber file is produced from. And when two sets of
Gerber files are set up in a (CAM) Configuration file, then there are
assorted implications when it comes to actually producing these Gerber

For starters, it will typically be the case that each set of Gerber files
will use a different set of embedded apertures (assuming that the RS274X
option is selected). And the first file to be produced that lists the set of
apertures used (with the corresponding set of Gerber files) will be
overwritten by the second file of the same nature, that lists the (typically
different) set of apertures used with the corresponding (other/second) set
of Gerber files.

>From my recollections, a report file that is produced at the same time as
the first set of Gerber files is similarly also overwritten when the second
set of Gerber files is subsequently produced (by an updated version of the
report file).

In the circumstances, my inclination would be to deselect the RS274X option
and invoke the feature in which an aperture list is created whose contents
are determined by the contents of the PCB file. Then I would use that
aperture list when subsequently generating the Gerber files. The resulting
Gerber files would be of RS274D nature (no embedded aperture definitions),
and an aperture file would be produced for each Gerber file produced.

Because all of those aperture files have identical contents, it is not
necessary to retain more than one of those files. And although I have not
had cause to use it "in anger" yet, I have written a Perl script which will
parse the contents of the aperture file, and then add appropriate embedded
aperture definitions to all of the Gerber files, so converting them from
RS274D format to RS274X format.

Although this sounds convoluted, the outcome of doing this is that *all* of
the Gerber files use the *same* set of embedded apertures. (Theoretically, a
PCB manufacturer should be able to handle different Gerber files using
different sets of embedded apertures. But my preference would be to not push
my luck. And I consider that it is probably easier to preview a set of
Gerber files when all of them use the same set of embedded apertures.)

Before the release of the CAM Manager server, users could control whether
Gerber files were of RS274D format or RS274X format, and regardless of how
the aperture list was determined (whether by the user or by Protel, based on
the PCB's contents). But as I have mentioned in earlier postings (the last
time was some time last year), there has been some loss of functionality
with the CAM Manager wrt Gerber file generation. The status quo is that if
you specify a set of apertures, then the Gerber files produced from these
will always be of RS274D format (no embedded aperture definitions); that
remains true even if the set of apertures concerned was created by Protel,
based on the PCB's contents. OTOH, it is possible to create RS274X format
Gerber files, but only if you forsake all control over which apertures are
used in these files. And in the event that different Gerber files
incorporate different sets of Mechanical layers, then it is likely that
different Gerber files will use different sets of embedded apertures.

That is not the only grumble that I have about the CAM Manager server, and
it is not necessarily the biggest shortcoming associated with it. But what I
have written in this post is something to be kept in mind in the event that
the contents of one or more Mechanical layers are to be included within only
*some* of the Gerber files produced.

Geoff Harland.
E-Mail Disclaimer
The Information in this e-mail is confidential and may be legally
privileged. It is intended solely for the addressee. Access to this
e-mail by anyone else is unauthorised. If you are not the intended
recipient, any disclosure, copying, distribution or any action taken
or omitted to be taken in reliance on it, is prohibited and may be
unlawful. Any opinions or advice contained in this e-mail are
confidential and not for public display.

* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *
*  This message sent by: PROTEL EDA USERS MAILING LIST
*  Use the "reply" command in your email program to
*  respond to this message.
*  To unsubscribe from this mailing list use the form at
*  the Association web site. You will need to give the same
*  email address you originally used to subscribe (do not
*  give an alias unless it was used to subscribe).
*  Visit http://www.techservinc.com/protelusers/subscrib.html
*  to unsubscribe or to subscribe a new email address.
* * * * * * * * * * * * * * * * * * * * * * * * * * * * * * *


To leave the EDAFORUM discussion list, send a email with
'leave edaforum' in the body to '[EMAIL PROTECTED]'

More Information : http://www.dolist.net

Reply via email to